topic Re: How to change aproaching feed for cycles in PowerMill Forum

How to change aproaching feed for cycles

Anonymous — Mon, 13 Jan 2020 08:27:28 GMT

Hello,

The programs goes to cycle start position at full speed, we would like to limit the approaching feed rate.

Right now it looks like in example below @:

19 TOOL CALL 41 Z S6700
20 L M03
21 ; PARAMETRIC FEEDRATE DEFINITION
22 Q1=300; PLUNGE FEED RATE
23 Q2=400; CUTTING FEED RATE
24 Q3=3000; SKIM FEED RATE
25 Q4=8000; RAPID FEED RATE
29 L X+0.0000 Y+0.0000 FMAX
30 L Z+50.0000 R0
32 CYCL DEF 208 BORE MILLING~
Q200= 0.25; SET-UP CLEARANCE~
Q201= -1.07; DEPTH~
Q206= Q2 ; FEED RATE FOR PLUNGING~
Q334= 0.05; PLUNGING DEPTH~
Q203= -27.1063; SURFACE COORDINATE~
Q204= 77.1063; 2ND SET-UP CLEARANCE~
Q335= 20.306; NOMINAL DIAMETER~
Q342= 20.306; ROUGHING DIAMETER~
Q351= +1; CLIMB OR UP-CUT
33 L X+0.0000 Y+0.0000 R0 FMAX M99

We would like to add the line in posprocessor that will allow us to go at limited feed let say F6000 to CYCLE start point, and then call a cycle

Re: How to change aproaching feed for cycles

barr.jarryd — Fri, 17 Jan 2020 15:07:41 GMT

Hey there.

At the end of your program start block for the post processor you can change the FMAX setting to a manual input.

Just double click on the post block and type in the desired speed you wish to run the approach at.

Hopefully this helps.

Re: How to change aproaching feed for cycles

Anonymous — Wed, 29 Jan 2020 17:52:35 GMT

A. Restrict FMAX to 6200 on Z-axis (Dangerous for advanced users only):

B. The same with NC program executing:

BEGIN PGM tst MM 
; Z axis FMAX=6000
FN 17: SYSWRITE ID1000 NR1010 IDX2=+6000
.
.
.
.
; Restore Z axis FMAX=10000
FN 17: SYSWRITE ID1000 NR1010 IDX2=+10000
13 END PGM tst MM

For Access FN 17 function:

C. Modify PP:

Create User Defined Parameter "Drilling Clear Plane Absolute", then

Re: How to change aproaching feed for cycles

Anonymous — Wed, 05 Feb 2020 08:46:17 GMT

Thank you very much karbidhegyu

I used solution "C" and it works very well

Re: How to change aproaching feed for cycles

Anonymous — Tue, 11 Feb 2020 07:47:37 GMT

So I used option C.

And one thing is not perfect in that solution,

Because Z value is now Drilling Clear Plane = Drilling Clear Plane + Drilling Hole plane

It is looping over if we have multiple holes, I am not so sure how to solve that,

I tried to make my own parameter to stop looping User Par = Drilling Clear Plane + Drilling Hole plane

But it seems like you cannot use expression in user parameters. Do you have any idea how to come over it ?

Thanks

Re: How to change aproaching feed for cycles

Anonymous — Tue, 11 Feb 2020 07:52:25 GMT

I found the solution, I found the parameter called ' Drilling user Parameter' and I utilized it.